Finite Element Analysis (FEA)

Introduction:

In order to determine the response of the spacecraft to various environments, a Finite Element Analysis (FEA) of CubeSat is required. One of the most critical conditions that the CubeSat will experience is the launch environment. This is the time from when the satellite leaves the surface of the Earth and reaches the desired orbit. During the launch time, the CubeSat will experience various vibrational loads from the launch vehicle.

The CSA requires the following structural model and analysis from the Mechanical subsystem at CDR.

· Structure Finite Element Model – Model checks

· Modal Analysis – estimation of the first mode

· Quasi-Static and Random vibration

· The margin of safety – Material, Joints (bolted, bonded)

Finite Element Analysis Procedure:

In order to obtain the results of the FEA, a few steps must be taken from the CAD model.

1- Simplification:

Since the CubeSat’s CAD model contains lots of detail, it will be very difficult to run a FEA on such a detailed model because of limitation in computational resources. Therefore, it is necessary to simplify the CubeSat model. It is important to optimize the simplification. It means that components with a crucial role in CubeSat structure and mission should not be simplified or slightly simplified. CubeSat’s structure is very important in its survival during the launch. Thus, the rails and each module’s shells will be not simplified in this analysis. Other internal and external components that have less effect on the analysis need to be simplified. Major simplification is done by assuming those components as lumped masses. Furthermore, mesh size has a great impact on FEA runtime. Thus, an average mesh size is considered for all components.

2- Finite Element Method (FEM):

The next step in the FEA process is to create the FEM model of each component. By using the 3D CTETRA element and different mesh size, the FEM model for each component of the CubeSat is created. Next, the lumped mass for each module is modeled.

3- Assembly FEM:

In this step, all the FEM models are assembled together. Then, bolt connections are defined for the whole assembly.

“Spider at Junction’’ as bolt connection type and “RBE2” as element type are chosen for all bolts connections in the CubeSat.

Figure 1: CubeSat's assembly FEM model

4- Simulation:

Prior to run the simulation, boundary conditions of the simulation need to be defined.

Contact:

First boundary condition is the contact between the components. “Surface to Surface contact” with friction coefficient of 1.04 is selected in this analysis.

Figure 2: CubeSat's contact model.

Constraints:

Second boundary condition to be placed on the CubeSat is the constraints. Since the CubeSat will be placed inside the NanoRacks deployer (NRCSD), the CubeSat is completely fixed along the z-axis. But, there is 0.5 mm gap between the CubeSat’s rail and deployer. Due to the difficulty of modelling this gap, one node at each top and bottom of the 4 rails is fixed along x-axis, and one node at each top and bottom of the 4 rails is fixed along y-axis. The boundary conditions used in this study can be found in the following table.

Structural Analysis:

In this section, the three analysis required by CSA and NanoRacks are done.

Modal Analysis:

The first analysis to be run is the Modal Analysis (Normal Modes Analysis). The purpose of this analysis is to determine the natural frequencies (normal modes) of the CubeSat. The natural frequencies are frequencies at which the CubeSat will get excited and large displacements of the structure will occur when the CubeSat is subject to a vibration [1]. The natural frequency can be obtained by the following equation.

where w is the natural frequency, k is the stiffness and m is the mass. The CubeSat large displacements can cause a lot of amounts of stress in the structure during the launch. By extracting the natural frequencies, we can prevent the CubeSat from resonance with the launch vehicle. There will be several normal modes, but only the first few modes are of interest. This is because, the first few modes have the largest displacements and therefore the largest stress. The NanoRacks requires that the first normal mode of the satellite be greater than 100 Hz.

Quasi-Static Analysis:

The CubeSat has to survive the acceleration loads during the launch. In order to determine the stress level on the CubeSat due to these acceleration loads, quasi static launch analysis are performed. According to NanoRacks, the CubeSat needs to provide positive margins of safety when exposed to the accelerations documented in Table 4.3.1-1(NanoRacks CubeSat Deployer Interface Definition Document [2]) of the item, with all six degrees of freedom acting simultaneously.

Figure 3: Acceleration loads on the CubeSat

Random Vibration Analysis:

During the launch, the NRCSD will induce vibrations onto the CubeSats. As demonstrated before, it was confirmed that the CubeSat has normal modes higher than what is required by NanoRacks. However, several vibrational loads will cause stress in the CubeSat during the launch phase. Thus, it is important to simulate the full launch environment and inspect stresses induced onto the CubeSat. If the stress is less than the yield strength of materials, then it can be confirmed that the structure will survive the launch.

The NRCSD's hard-mount configuration is chosen for this random vibration analysis. The hard-mount test profile can be found in the Table 4.

In this analysis, the same CubeSat model is used. Also, the random vibrational simulation has to be run on all three axis.

Table 4: Random Vibration Hard-mount Test Profile (Table 4.3.2.1-1 of NRCSD-IDD)

Results:

Modal Analysis:

After conducting the modal analysis for the CubeSat, it is found that first natural frequency is occurred at 442.495 Hz which meets the minimum requirement of NanoRacks (100 Hz). Also, Table 5 reveals the 15 first normal modes of CubeSat.

Figure 4: CubeSat's first mode displacement result.

Quasi-Static Analysis:

The CubeSat's quasi-static analysis result is shown in the following figures. It has a maximum displacement of 4.05E-5 mm,

Figure 5: CubeSat's displacement result of Quasi-static analysis.

and maximum stress of 0.353 MPa.

Figure 6: CubeSat's stress result of Quasi-static analysis (The deformation is shown as 10% of the model).

Random Vibration Analysis:

The random vibration analysis results are shown in the following figures. The obtained results demonstrate that the maximum von-mises stress on the CubeSat is found to be 1.943 MPa.

Figure 7: CubeSat's random vibration analysis results.

The CubeSat's structure is constructed of aluminum 6061-T6 which its yield strength is 276 MPa. The maximum stress was found to be 1.943 MPa, which is below the yield strength aluminum 6061-T6. Therefore, the structure will survive since it will not yield.

References:

[1] Furtal, Jude Joseph. "Structural Design and Finite Element Analysis of DESCENT CubeSats." (2020).

[2] Deployer NC. Interface Definition Document (IDD). NanoRacks LLC. 2018.

Conducted and documented by:

Ali Barari

Page updated

Google Sites

Report abuse